Part offset question

[l u k e]

Another newbie question, the Haas manual is no help so here I am (again). I'm a little confused on setting the “work piece” z height (Not the tooling).

I purchase the Pro Touch Off Gage>



I touched off all my tools with the Pro Touch off Gage sitting on top of my vice which will place the tools 4" above that point. My work piece will be below that, which seems to be the general consensus on how to do it.

What I'm unsure of is inputting the Z height of the work piece. I have two guesses on how to do it, but it's only a guess.

Guess #1
Would I just measure the difference in height between the “Z setter zero” and the top of the part, and then input that difference in the Z height for the work offset?
In other words if my part was going to be G54 and it happens to be exactly 2.2000" lower than the zero height on the z setter, would I would type in -2.2000 for Z in G54?

OR

Guess #2
The manual only has one suggestion on this and it is to touch off the tools to the top of the part, this leads me to my second guess.

Using the same scenario with my work piece being 2.2000 below my Z setter zero, would I simply edit the tools by adding 2.2000 to the measured height? (This doesn’t seem to be much of a shortcut using a z setter)

I just can’t figure out how else the control would know the relationship between the tool Z height and the part Z height.

[MSFAB]

I do the same thing all day long but use a 1 inch tool setter.
1st measure the distance from the top of the vice to the top of the part using the machine and a dial indicator. Insert that into the z value for g54 then minus the hieght of your tool setter.

Example
Difference between vice and part
+2.5
Tool setter 4.0
Enter 2.5 f1 Into g54 z value
Then -4.0 write enter button
You will get -1.5 for z offset
Then always check the first tool with a 123 block

Hope this helps
Then

Sent from my SAMSUNG-SGH-I897 using Tapatalk

[MSFAB]

Assuming your setting the tool setter on top of the vice if not measure from where ever the tool setter is sitting. I use a mitutoyo setter
Cheers
Marcus

Sent from my SAMSUNG-SGH-I897 using Tapatalk

[l u k e]

Originally Posted by MSFAB I do the same thing all day long but use a 1 inch tool setter. 1st measure the distance from the top of the vice to the top of the part using the machine and a dial indicator. Insert that into the z value for g54 then minus the hieght of your tool setter. Example Difference between vice and part +2.5 Tool setter 4.0 Enter 2.5 f1 Into g54 z value Then -4.0 write enter button You will get -1.5 for z offset Then always check the first tool with a 123 block Hope this helps Then Sent from my SAMSUNG-SGH-I897 using Tapatalk

So you're saying that guess #1 is correct, I just input the difference and don’t reset all the tools z height like guess #2 ??

[MSFAB]

Yes guess 1 is correct. The leave tools set where there at. What size Haas are you running?

Sent from my SAMSUNG-SGH-I897 using Tapatalk

[l u k e]

VF2

[MSFAB]

Hey Luke I took a short video on my phone so i apologize for the crappy resolution. I took it at work to show the process. The tool setter is to the left. I set the tools to that which is 1 inch.
I press the Mdi button then the hand jog button to zero the dro for measurement

YouTube - Haas mini z fixture setCheers Marcus

[l u k e]

I believe I understand the basics of the actual measuring; I was more inquiring about the “value” that was put into ‘G54- Z’ for the part height.

I have a Haimer 3D sensor that will remain in the tool changer on my machine.



I have set a tool height for the Haimer off the same block that I calibrated the Edge Z Setter with.



From the help I’ve received I’m under the impression that all I have to do is load the Haimer in the spindle touch off the Z height of my part; subtract the calibrated Haimer Z height from the part Z height put the difference in the Z setting for G54 (G54-G59 whichever I use).

The math:
'Haimer Z' -7.9404
'Part Z' -9.9549
'G54 Z control entry' -2.0145

Is that correct?

[MSFAB]

Yes that is correct. You got it.

Sent from my SAMSUNG-SGH-I897 using Tapatalk

[l u k e]

Sweet!

[Pondo]

Make sure setting 64 is "OFF" if you are touching off tools anywhere except the part Z0 surface.
If it is on, it will apply the G54 Z offset to the touchoff.
You have it figured out correctly. You can touch off tools on any surface, then put the G54 Z offset as the distance from that surface to the Z0 surface of the part. + or - does not matter. The controller adds that # to the tool offset position to figure out where the tool tip is when running a program.

[Pondo]

Another way to set the G54 Z0 is to use the Haimer to measure it. Just like you would with a regular indicator in the spindle.
Set the Haimer to 0 on the top of the 1-2-3 block where you have the red arrow and set the user Z display to 0.
Move the Haimer to set 0 on the part's Z0
The display Z0 is the G54 offset (the distance from the tool touchoff to the part Z).
You can use the Haimer (or an indicator) to measure very exact sizes in X and Y this way too, using the machine like a budget CMM.